SOLIDWORKS CAM - Waterjet, Plasma and Laser Cutting
With SOLIDWORKS CAM, all active subscription users get access to 2.5 axis part machining directly inside of SOLIDWORKS. This includes the ability to customize your SOLIDWORKS CAM to work with your Waterjet, Plasma and Laser Cutters.
Some things to consider when using SOLIDWORKS CAM for Waterjet/Plasma/Laser Cutting:
- Tool Setup
- Stock Material
- Machining Features
- Operation Plans
- Post Processor
Tech Tip: Consider this a quick setup guide and not a replacement for training and/or support. If you need help or get stuck in any one area, don’t hesitate to contact your local VAR.
Step 1: Customizing the Technology Database
The TechDB is used by SOLIDWORKS CAM to store everything from your custom machine and tool information to your materials and feeds/speeds.
To edit the TechDB, you can either launch it from SOLIDWORKS under Tools > SOLDIWORKS CAM > Technology Database, use the Technology Database icon on your command manager, or you can launch it independently from SOLIDWORKS by navigating to C:Program FilesSOLIDWORKS CorpSOLIDWORKS CAM (x)TechDBApp.
The first thing we’re going to do is create a tool in the TechDB that can be used to replicate your cutter.
Tech Tip: In the top-right of the TechDB is a Metric and Inches toggle. The information stored in these are independent from one another and the default is driven by the units set in your SOLIDWORKS document.
Under Mill Tooling > Flat End Mill choose any existing tool and select Copy.
Fill out the information on your new custom tool where Tool ID is the name of the tool and D1 will be used as the cutting diameter. Don’t forget to add your preferred Feed Rate settings as we will be passing these values to the post processor.
Click “Save” to add the information into the TechDB.
Next, we need to add our new Tool to the appropriate Tool Crib.
Select Mill > Tool Cribs and either create a new Tool Crib or use an existing. I will be adding this tool to Tool Crib 2.
Select Add > Flat End Mill.
Find your newly added tool and hit the Select button in the top left.
Step 2: Stock, Setup and Feature Definition
Open the part file to be used for machining and activate your CAM Add-in via Tools > Add-ins > SOLIDWORKS CAM.
Right-Click Stock Manager and select “Edit Definition”.
Tech Tip: It is recommended to keep the depth of stock equal to the thickness of the part. For most operations, Z-Height is critical and can be controlled via the post-processor or edited manually after the post is created.
Make sure you add enough stock material around the part to work with. You can match the exact stock size if desired.
Create a Mill Part Setup on the top face of the part. This will determine your machining direction.
Right-Click Mill Part Setup and add a 2.5 Axis Feature.
Set the Feature Type to Pocket and the Selection Filters to Inner Loops and Convert to Loop. Then select the top face. These settings will ensure that all inner cuts will be collected with one selection.
Move to the next step in the Feature Definition by selecting End Condition.
Set the Strategy to a single operation plan such as Finish, and set the End Condition direction to Up To Face by selecting the bottom face of the part.
To create the perimeter cut, create a new 2.5 Axis Feature but this time, select the type as a Boss and change the selection filters to Outer Loop and Convert to Loop and then select the outer edge of the part.
For the End Condition, select “Up To Face” and select the bottom of the part just like we did in the previous 2.5 axis feature creation.
Generate all Operation Plans.
Step 3: Optimize Machine Parameters
If any operations are not using the newly created 1MM Plasma tool, you can navigate to the SOLIDWORKS CAM Tool Tree and drag and drop operations onto the correct tool.
Since all operations will be using the same machining parameters, we can also combine them all on the SOLIDWORKS CAM Operation Tree to make them easier to edit.
Select all of the Contour-Mill operations, right-click and select “Combine Operations”.
Right-Click Contour-Mill1 and select “Edit Definition”.
To use the feeds and speeds defined in the tool creation, navigate to the feeds/speeds (F/S) tab and set the Defined by to “Tool”.
Next, we need to set the number of passes to 1 by changing the Depth Parameters on the Contour tab.
Tech Tip: Typically, the depth will be determined by the max cutting depth allowed by the cutter. However, to ensure we only have a single pass we are setting the depth to be larger than the material thickness.
We also need to set the Final Cut Amount found under Settings on the Contour tab.
Be sure to check your Leadin and Leadout values on the Leadin tab.
By checking “Apply Leadin/out to All”, you can change the values for all operations at once.
Finally, run Simulate Toolpath to verify your toolpaths are correct.
Tech Tip: Depending on how the model was designed, you might want to look into Tab Cutting for holding the part in place during and after machining.
If any toolpaths do not look correct, return to Edit Definition on the Contour-Mill operation and change settings as needed.
Step 4: Post-Processing
The last process is to post to the machine, SOLIDWORKS CAM includes multiple posts, however they are not guaranteed to work for your machine so make sure to run tests on any post you have not used before.
And as a final note, we can always help create a custom post for your machine also, so please don’t hesitate to give us a call.
Computer Aided Technology, LLC.